November 2010

11/16/2010

By clicking into the Equation column, we can overwrite any of the current values. If the overwrite affects the size in the model, we will be able to see the change immediately.

Next we will modify the model parameters with the values in the table below.

Name

Equation

Description

FTh

8

Floor Thickness

LenA1

SIL + (2 * WTh)

2D Distance 1

LenA2

SIW + (2 * WTh)

2D Distance 2

LenA3

18

2D Distance 3

LenA4

18

2D Distance 4

LenB1

SRS + FTh

3D Distance 1

SBSH

SRS + FTh

Structure Height

SBSL

SIL + (2 * WTh)

Structure Length

SBSW

SIW + (2 * WTh)

Structure Width

SIL

32

Inner Structure Length

SIW

32

Inner Structure Width

SRS

40

Rim to Sump Height

SVPC

18

Vertical Pipe Clearance

WTh

8

Wall Thickness

Although it appears that SIL, SIW, and SRS are constant according to the table, under size parameters, we will configure SIL and SIW to refer to a list of values. SRS will always inherit the depth calculated between the surface and the floor of the structure once the structure has been inserted into a pipe network.

Next we configure Size Parameters. Think of this step as setting the properties of each Model Parameter.

There are three views we can set for size parameters:

Edit Configuration

Edit Calculations

Edit Values

If we first go to Edit Configuration, we can check out the values for Data Storage. Each parameter that was configured with an expression has its Data Storage setting configured to Calculation. Each parameter that was configured with a numeric value has its Data Storage setting configured to Constant. We want to reconfigure that setting for SIL, SIW, and SRS.

Start by clicking on the Data Storage value for SRS and setting it to Range. Click on the Data Storage value for SIL and set it to List, then do the same for SIW. Next change the view to Calculations.

Edit the SIW value. Here is where additional sizes can be added to this parameter's list. The same can be done for the SIL value.

Edit the SRS value. We configured this to be a range value so that we could specify minimum and maximum allowable depths for this structure. Remember that this actual value is calculated when the structure is added to the pipe network.

By setting the parameters, we are instructing the part how it determines size. We can assign values that are constant, calculated by an expression, or selected from a list. If you expand the Model Parameters section on Content Builder, we can observe a list of parameters that must be configured in order to get our part working.

Junction structures have certain predefined parameters that must be understood. Let's look at some common parameters:

Back in our model, if we set our view to SW Isometric, we'll have a great vantage point for the extrusions we are about to create.

Next we will apply an extrusion to create our box. We will extrude 48 units away from the Top Plane in the downward direction.

Since we are creating this extrusion at a given distance this will be a blind extrusion. We fill in the check box for Flip since we are extruding in a direction away from us relative to the plane instead of towards us.

Next, we will add a model dimension to define the depth of the box.

Select the extrusion then pick a general location for the dimension line.

The Placement Point will appear as a small cyan circle when we save our part. If it does not appear, close and then reopen the part.

If we set our view on the Top Plane, we can relocate the Placement Point to the constrained location with our endpoint osnap.

In our current work plane, the top plane, we want to add dimensions so we can control the length and width of this structure. We also want to add dimensions to further constrain our placement point.

The length measurement of the structure will be assigned by a horizontal distance dimension. We can place this dimension by selecting the two points coinciding at the endpoints of the top line. The value of this measurement will be 48. After placing this dimension, notice

The width measurement of the structure will be assigned by a vertical distance dimension. We can place this dimension by selecting the two points coinciding at the endpoints of the left line. The value of this measurement will be 48.

We can dimension the smaller box in the same manner using 18 as the value for the horizontal and vertical distance dimensions.

When we apply modifiers, we are modifying the profile from a 2D shape to a 3D feature. There are a few ways to do this:

Extrusion: The profile is swept or projected from its work plane for a distance or to a location relative to another work plane.

Transition: The profile is swept or projected to meet another profile that may differ in either size or shape.

Path: This is like a transition if you think of one shape sweeping into another shape. However, this modeling occurs in one work plane. The two profiles are created as "samples" in the current work plane. Then a line or arc is drawn in the work plane which represents the path that the first profile transitions into the second profile. The profiles placed on opposite ends of the segment transverse to the work plane and the transitioning occurs as illustrated below.

Boolean Add: Groups more than one modifier together to create one object.

Boolean Subtract: Deducts one or more modifiers from the overall object.

Cut Plane: Maybe cut planes worked in a previous release or another vertical but not in Civil 3D's Part Builder.

After you apply a modifier, it is important that you add a model dimension to the direction of the extrusion. Model dimensions, like work plane dimensions, will be related to model size parameters therefore enabling the part to resize when necessary.

When the first model dimension is placed, the Placement Point then appears. At this time we will osnap that point onto the planned location we constrained earlier.

11/07/2010

There are two types of dimensioning we can apply in Part Builder: work plane dimensions and model dimensions. We will look at model dimensioning when we discuss Apply Modifiers. The commands for work plane dimensioning are available on the right click menu of the work plane.

The purpose for applying dimensions in Part Builder is a bit different then then the reason why we apply dimensions in AutoCAD. Dimensions in AutoCAD display measurements. Dimensions in Part Builder are responsible for causing aspects of the part to resize and for defining measurements usually in terms of parameter values. Dimensions can only be applied to AECCU_COL_GEOMETRY objects. The types of dimensions we can define are:

Distance: Defines the distance measurement between any two objects. This measurement can be at any orientation. You will be prompted to select two entities and then the location of the dimension line. The actual measurement from the model will appear in the dimension. If you edit this dimension and change its value, you will cause a size change in the model.

Horizontal Distance: Same as a distance dimension but the dimension is constrained to a horizontal orientation in the work plane. However, unlike the distance dimension, you are prompted for a distance value before the command exits. If you specify a value different than actual, you will cause a size change in the model.

Vertical Distance: Same as a horizontal dimension, but the dimension is constrained to a vertical orientation in the work plane.

Parallel Distance: Defines the distance measurement between any two objects. You will be prompted to select two objects to dimension and then for a reference line. The dimension line will be oriented parallel to the reference line.

Perpendicular Distance: Same as parallel dimension, but the dimension line will be oriented perpendicular to the reference line.

Diameter: Measures the diameter of a circle. The actual measurement from the model will appear in the dimension. If you edit this dimension and change its value, you will cause a size change in the model.

Angle: Measures the angle between two converging lines. You will be prompted to select two lines and the location of the dimension arc. You will then be prompted for the measurement of the angle in degrees before the command exits. If you specify a value different than actual, you will cause a size change in the model. Note, as unusual as this may seem, if the lines do not meet at their endpoints, this dimension may change your geometry.

Next we will see how applying dimensions will benefit our current modeling project.

11/03/2010

At this point in time in the Part Builder workflow, I setup the location for the "insertion base point" for the structure. This is referred to as the Placement point. The location of this point also determines where the pipes will converge at the structure. This is done by creating two perpendicular lines running from the edge of the structure to this location. Since we created the rectangular profile using the "quickie" command, no further restraints are needed for this geometry.

In this example, this point will be located 18 units to the right of the top left corner and 18 units below.

Right click on the Top Plane and select Add Geometry>Line.

Create two lines as shown in the illustration below:

The following constraints will be applied:

Each line will be perpendicular to the larger line attached to.

Each line will be perpendicular to each other.

Points coinciding with the larger lines will be coincident to those lines.

Finally, expand Top Plane>Geometry section in Content Builder. Select the point representing the Placement Point for the structure. Notice that the point in the model area will auto-preview when selected. Right click and select Fix to lock the location of this point.

The Placement Point definition can be finished after modifiers such as extrusions or transitions have been created. Therefore, we will wrap up defining this point during the Apply Modifiers part of the work flow.

When we constrain, we fix geometry and relate its orientation and position to other geometry in a particular work plane. This ensures appropriate behavior when geometry resizes. Certain constraints are automatically applied.

When creating line or arc geometry using the Content Builder, points are placed at endpoints along with coincident constraints which keep the point and end of line always in the same location.

When creating rectangular profiles, coincident constraints are placed where the endpoints and points coincide and perpendicular constraints are placed on the lines forming corners.

When oval profiles are created, parallel constraints are placed between the two parallel lines, tangent constraints are placed where the arcs and lines intersect and coincident constraints are placed on endpoints and points.

We can also apply constraints manually when we create custom profiles. The following constraints are available:

Tangent - Maintains tangency between two arcs, or an arc and a line.

Parallel - Forces two lines to remain parallel.

Perpendicular - Forces two lines to remain perpendicular

Concentric - Maintains location of a point at the center of an arc or circle. Will also force arcs and circles to maintain the same center point.

Coincident - Forces two types of geometry to occupy the same position.

Equal Distance - Maintains an equal distance between three points.

Equal Radius - Maintains an equal radius between arcs and circles.

Midpoint - Forces the position of a point to be equidistant between two lines.

Symmetric - Maintains symmetry about a line.

Normal - Forces a curve to intersect a line or curve where its tangent is perpendicular.